Weldment help 2

[LesPaul82]

I am trying to create structural member weldments for our company. Looking at the default ones that Solidworks provides, it seems to be just a sketch saved as a '.sldlfp' Library Feature part. So I drew a sketch of a W6"X15# and saved it as a '.sldlfp'. But when I try and use it when creating a weldment, it says that the library feature is empty. I can't figure out what else I need to do to the sketch.

Sean Nutley
Carmanah Design and Manufacturing
Vancouver, BC, Canada

http://www.carmanahdesign.com

 

[MElam]

The easiest thing to do is take the profiles that came with SWx and do a save-as or copy them, then edit the sketch. You could copy the s section folder to make w profiles. You will have to edit the custom properties of the library feature to get the description correct in the cut list.

 

[SBaugh]

To get the Weldment Profiles to work, all you need to do is make a new part with a single sketch of the desired profile. A good tip is to include several points in the sketch to give yourself many options to locate the profile when you make Weldments.

1) Select the sketch in the FM and go to FILE/SAVE AS/Library feature part.

2) Now, put this *.sldlfp into a folder that has a couple levels. For example, I made a folder called CUSTOM WELDMENT PROFILES/EXTRUDED ALUMINUM/INCH/ and placed the *.sldlfp in the INCH folder.

3) Now go to TOOLS/OPTIONS in SW and choose the File Locations category......then Weldment Profiles, then browse to the CUSTOM WELDMENT PROFILES folder.

4) When you use the Weldment Tool, you will now see an additional STANDARD called EXTRUDED ALUMINUM, a TYPE called INCH and a SIZE called whatever you named your *.sldlfp.

5) Of course, your folder names will differ, but the depth of the nested folders is VERY important for them to show up in the tool correctly.

Regards,


Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[LesPaul82]

Didn't even think of that. Thanks a lot. I just found out that you can make a profile, exit the sketch, save the file as a '.sldlfb' then right click the sketch in the tree and click 'Add to Library'.

Sean Nutley
Carmanah Design and Manufacturing
Vancouver, BC, Canada

http://www.carmanahdesign.com